Cadence® system design and verification solutions, integrated under our System Development Suite, provide the simulation, acceleration, emulation, and management capabilities.
System Development Suite Related Products A-Z
Cadence® digital design and signoff solutions provide a fast path to design closure and better predictability, helping you meet your power, performance, and area (PPA) targets.
Full-Flow Digital Solution Related Products A-Z
Cadence® custom, analog, and RF design solutions can help you save time by automating many routine tasks, from block-level and mixed-signal simulation to routing and library characterization.
Overview Related Products A-Z
Driving efficiency and accuracy in advanced packaging, system planning, and multi-fabric interoperability, Cadence® package implementation products deliver the automation and accuracy.
Cadence® PCB design solutions enable shorter, more predictable design cycles with greater integration of component design and system-level simulation for a constraint-driven flow.
An open IP platform for you to customize your app-driven SoC design.
Comprehensive solutions and methodologies.
Helping you meet your broader business goals.
A global customer support infrastructure with around-the-clock help.
24/7 Support - Cadence Online Support
Locate the latest software updates, service request, technical documentation, solutions and more in your personalized environment.
Cadence offers various software services for download. This page describes our offerings, including the Allegro FREE Physical Viewer.
Get the most out of your investment in Cadence technologies through a wide range of training offerings.
This course combines our Allegro PCB Editor Basic Techniques, followed by Allegro PCB Editor Intermediate Techniques.
Virtuoso Analog Design Environment Verifier 16.7
Learn learn to perform requirements-driven analog verification using the Virtuoso ADE Verifier tool.
Exchange ideas, news, technical information, and best practices.
The community is open to everyone, and to provide the most value, we require participants to follow our Community Guidelines that facilitate a quality exchange of ideas and information.
It's not all about the technlogy. Here we exchange ideas on the Cadence Academic Network and other subjects of general interest.
Cadence is a leading provider of system design tools, software, IP, and services.
how to generate spice netlist without some subckt, as following:
the default netlist as following:
R1 net1 net2 10k
Xnosubckt in1 in2 out1 opamp
.sunckt opamp in1 in2 out
But I need no subckt netlist, as following, How can I get this? I set property like "nlAction" ,in subckt, actually there is nothing ,but I also need there is no ".sunckt......" How Can I get this ?
I need something like this
thanks a lot
Hi Hanlei I am not very clear on the question so there is some guessing here. Please correct me if I am wrong. I think you would like to have a spice (or maybe spice-like) netlist with only the instance lines and not the subckt definitions.You can do this with cdlout as follows:a. In the library manager, copy the symbol view of cell "opamp" as "auCdl" viewb. In ciw, go to "File->Export->CDL"c. Fill in the fields accordingly and press OK buttonYou will only get the instance line for cell opamp and not the subckt definition. Hope that this is what you need. : ) By the way, when posting a question, it would be great if you can provide the version info so that we can come up with the best solution for you.E.g.unix>virtuoso -Wunix>icfb -Wunix>spectre -WBest regardsQuek
In reply to Quek:
My systerm info. as following:
icfb : 184.108.40.206
Thank you for your solution at first. My systerm is IC 5.1.41, I tried you solution , it works. but I need netlist format is HspiceS format, and I generate netlist from Analog Design Environment, so does there is any other options? I had used "nlAction" 4 years ago, but this time it does not works, maybe the version has difference.
In reply to hanlei1975:
Hi HanleiI am a little confused. I think adding "nlAction=ignore" on an instance will prevent it from appearing in the netlist, not even the instance line. This should not be what you are looking for. I have found an obsolete solution #1835032 which might be what you need. Here is what you have to do:a. Copy the symbol view of your opamp as "hspiceS" viewb. Edit the cdf property of opamp cell to include a string parameter named "macro"c. Enter the name of the subckt as the macro value, e.g. "opamp"d. In simInfo section for hspiceS, enter "macro" for "otherParameters"e. In "Setup->Environment" of ADE, enter the path to the file containing the subckt defintionf. Netlist using hspiceS. It should work nowBy the way, perhaps it is time to upgrade to the latest IC614 or IC5141. Your version of spectre is also very out-dated. : )Best regardsQuek
you are right, I got it. Thank you very much!
one more question, I had done as you wrote a~f , but the netlist like:
XI0 net1 net2 out opamp_opamp_G36
actually, my subckt named opamp, so when I do simulation use netlist, the simulation does not work. I need to modify the netlist,change "opamp_opamp_G36" to "opamp, the simulation can work, so can wen generate the netlist like:
XI0 net1 net2 out opamp
Hi Hanlei, Quek,
Actually it is possible to do this.
Add a CDF parameter called "macroArgumentStyle" with value "include" (anything other than "default" or "USE") and then the call should not get mapped - and it will also not complain about not being able to find the file macro.s (where macro is the name of the macro parameter).
Again, this was in an old (now obsolete) solution. hspiceS (and all socket simulator interfaces) are long obsolete, and as such much of the information about how to customize the netlister has gone. hspiceS is no more after IC5141.
In reply to Andrew Beckett:
Hi AndrewThanks. : ) All the best for 2010. Best regardsQuek
Hi Andrew, Quke
Problem was solved by your help.
thanks a lot
Happy new year! :)